Hotrod for Solidworks

[jackboot]

Does anyone have any suggestions for speeding up Solidworks?

I am running dual 3.06 Ghz processors, 7110 Wildcat Graphics card, 4 Gig of Ram, and I have a hugh hard drive.

We have assembly's with complicated features and threads. Solidworks has always been slower than Pro (my experience only and I don't want to debate this topic) but while we will see speed increases from new releases - we never seem to get to a point where we are doing work in a quick manner.

So - any tweaks, ideas, suggestions...anyone have an idea?

jackboot

 

[TheTick]

RE: "...we never seem to get to a point where we are doing work in a quick manner."

You mean you spend too much time waiting for rebuilds? Or is this a proficiency issue?

Good and evil: wrap them up and disguise it as people.

 

[jackboot]

I consider myself and everyone in my department experts in Solidworks- so yes rebuilds.

We wait on the machine to grind through rebuilds- typically this will be the biggest headache on assembly drawings and assemblies themselves.

Additionally, I know about configurations and envelopes - but we will always come to the point where we have to "open it up" for the final work.

I am just looking to see if anyone has found a way to push Solidworks faster.

 

[Rocko]

Tick,
That brings up a good point what do you think someone can do to help speed up rebuilds on a part.

 

[TheTick]

Sorry, I tend to lapse into skeptic mode sometimes. I know SW can be slow.

I have a second physical hard drive that I use for swap space. I've never really experimented to see how much that helps. It does help with NASTRAN.

What about the rest of the hardware? RAM bus speed? RAM speed? Clock? Some of these questions might best be posed in a hardware forum.

I know dual processors are no help.

Curious as to why you are modeling actual threads. I know helixes really dog things. I do a few torsion springs, and they are inordinately slow.

If helical surfaces are your problem, you may want to try to find a way to simplify the geometry with an approximation.

Every CAD system has its limitations. Even UG ran into trouble with some things, and we were forced to modify our work habits (partial assemblies, etc.) and tough it out with the final regenerations.

Ultimately, SW is and always shall be mid-range CAD.

Good and evil: wrap them up and disguise it as people.

 

[LoveAeris]

How about creating an assembly cut?

Suppressing some parts or assemblies doesn't work well because sometimes you get bunch of mating error. Instead, just draw a big enough box where you don't have to see and cut through. It will reduce rebuilt time and also file size as well. Whenever you want to see everything, you just suppress the cut.

 

[jackboot]

While I am not a computer expert - I know that the RAM, RAM speed, and everything else that is spec'd into our machines is the absolute fastest money can buy. I usually email David Schaller who does the bench marks for Solid Solutions Magazine to get the scoop on the lastest and greatest hardware before ordering a machine.

The dual processors have a very limited effect on the rebuild times (Solidworks is not set-up to take advantage of this nor is it set-up to take advantage of the 64-bit technology). However, two processor allows a couple of things to happen at once - I can run other programs while Solidworks is grinding away - answer email - the usual stuff. I do wonder though, I will peg both processors on regens of drawings - so they will work together on certain things.

Threads - we have always had them. They look cool and make a good drawing. Also, the threads allow us to check thread reliefs for machinists and verify certain machining details - but this is nick picking stuff. The threads are there because everyone likes to see them. When we took them off there was an outcry - so it became the de facto standard.

I had some serious issues with Pro - things they would not address. We had to go to Solidworks.

jackboot

 

[SBaugh]

Well since your company requires you to have real threads and you can't simplifiy your models your kind of SOL. A single helix can hurt the performance of any machine. When you have multiple helixes being used in an assembly, then your going to take a performance hit no matter how awesome your computer is. So if you can't simplify your models there really isn't anything anyone can do or suggest. I might over looking something here...but I don't think so.

You could try and increase your Virtual memory space or if your working over a network, you can try moving them to your HDD and work from there. A network will slow you down even more. Besides you have huge HDD .

Run a search in this group on networks. There have been plenty of discussion on those.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
When in doubt, always check the help

 

[TheTick]

How about simplifying the threads as a stack of patterned revolves?

-or-

Make a one-revolution helix and pattern in the direction of the helix axis.

Good and evil: wrap them up and disguise it as people.

 

[jackboot]

I have heard that Solidworks is working on speeding up the threads - so maybe the gripes are reaching the folks up on top. But - I hate to even say this - Pro never had a problem digesting threads. What would be the difference between the two? Meaning - why would Pro handle it so well and Solidworks not well at all?

*** I love Solidworks- so please don't think I am picking a fight with the Solidworks users.****

I am only asking the question and not trying to sound like a disgruntled louse.

jackboot

 

[jackboot]

Good idea - but would a pattern be any faster? The resulting geometry would still be the same.

I will give it a shot and see.

P.S. "The Tick" was my favorite cartoon - shame it was cut.

 

[TheTick]

That many helical sweeps really is asking a lot of SW. I think part of the problem is that deep down SW is not a complex surface modeler. It can tough it out, but it does not have the same internal workings as UG or Pro/E or CATIA that allow them to speed through the swoopity stuff.

Also, I must apologize for the tone of my initial post (2nd eng-tips apology today). Tick is not having a swell week. I do try not to pollute this wonderful forum with my attitude-du-jour when it happens to be negative.

Good and evil: wrap them up and disguise it as people.

 

[MadMango]

[blue]Jackboot[/blue], I'll throw out a few suggestions.

1. Use Local Patterns of hardware models in your sub-assemblies. They seem to be faster than multiple instances of hardware.
2. Create simplified configurations of your hardware without the helix-based threads. Use these in the "installed" config of your sub-assys, and when you do exploded views, use the fully threaded models.
3. Stress the importance of "functionally acturate" models over "cool & pretty" models. The time you are waiting for rebuilds can be equated to a gernal dollar amount. Do a simple study, and it should be evident your ROI on not making fully threaded models will be huge.

MadMango
"Probable impossibilities are to be preferred to improbable possibilities."
Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[jackboot]

No problem - I didn't take as such and didn't mean to convey an attitude with my response.

We are constantly pushing the limit with what we use. Threads are bad, but we have several helical gears with the teeth modeled - in 1000 plus part assemblies. Our network was upgraded to giga-bit speed so we could do what we do. Opening these assemblies turns my hair grey.

Plus we have the Pro versus Solidworks debate all the time - I don't reget the switch (slow or not). Solidworks has a better creation logic and is much quicker in certain aspects. It can't do everthing Pro could do but what it does do is so much easier.

Plus - Solidworks is constantly working on improving the product - we will see the day that it will smoke along like it should.

 

[TheTick]

I just tried the pattern thing and it was S-L-O-W-E-R. Geometry pattern wouldn't take.

Honestly, that was a bit o' SW folk wisdom I once heard and never tried until now.

Good and evil: wrap them up and disguise it as people.

 

[SBaugh]

I have an example of the revolve linear pattern (for threads) at my site.

http://www.scottjbaugh.com

I know those are faster than true threads. Helical Gears are different, there isn't much you can do with those, except deal with...and use lots of hair dye .

I really hope they do improve the speed it takes to crunch a helix. That would save lots of people lots of time. Plus that would mean I can get my braided hose back out. It presently takes over 30+ minutes to load that part..yes a part takes 30 minutes to load. I have almost (i think) 20 helixes in it.

*** I love Solidworks- so please don't think I am picking a fight with the Solidworks users.****

I never thought you were, but if you turn on us and become a Pro-E user we will have to ...just kidding.

Best Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
When in doubt, always check the help

 

[lmcchesney]

If your gears and/or fasteners are standard parts that you are not likely to edit in the future, you can export them as parasolids and re-import them back into SW. The file sizes drop by about 2/3 with the consequent performance improvement.

 

[jackboot]

Thanks for the information - everyone.

The export idea may save considerable time.

Thanks Scott I have marked your site in my favorites.

 

[maxmwiz]

One of things we use for graphics design speedup is four hard drives on one controller card. It allows much faster r/w times. I don't know for sure if this mirroring trick will work in the solidworks world.

 

[EdDanzer]

We use configurations on our fasteners, these models have mating geometry defined before any solid model is built so the first configuration can be used for interference detection, the second configuration has no threads and is the smallest file size and fastest loading, and last has cosmetic threads that are a revolved cut. The nuts have the same revolve cut threads on the inside. These revolve cut threads look good in parts manuals and are pretty fast to load. We have one 1500 part assembly with over 100 fasteners in it loads in a few minutes.
We have seen machines with too much RAM in relation to cache run slower than machines with less RAM. Test the machine with 10 time as much RAM as cache and see if the load times improve.